how to move body so edge is parallel to another 3d edge?

[maker9876]

I've inserted a rectangular component into a file and would like to position it so that one of its edges is parallel to the edge of a component that is already in the workspace.

Can't figure out how to do this at all?

[g-andresen]

Hi,

export file > save as f3d > attach to your next post for better understanding.

günther

[maker9876]

OK file attached.

In the image below we see the grey box that was already in the file, the green object which was inserted but which is at no particularly useful orientation to the box.

The question is, how to make the edges - indicated by the two red arrows - parallel to each other ?

[g-andresen]

Hi,

try it this way:

1. create component from body

2.  create rigid joint using "controlpoints"

regards

günther

[maker9876]

That works, thanks a lot!

Do you think that is the only way to do it?

In the past have had problems using Joints to position (or align) things in a design because joints can become corrupted.

If that happens then the whole design can "fall apart". Particularly if other objects were created by projecting items that had been positioned using a joint. So now try to get things correctly positioned using MOVE commands and then afterwards create the joint.

[maker9876]

I guess after the Joint command one could use a Move command to achieve the final alignment and then a Capture Position. At that point the Joint could be deleted and would be no longer relevant to future operations, no longer a part of the timeline.

[g-andresen]

Hi,

here is a positioning example:

The move command is not needed for changing position > edit joint is your friend!

For me, the joints are the only real thing.

günther

[maker9876]

Yes, I agree joints are a really nice way of positioning - and re-positioning - things. 

Really like to do that in CAM when laying out parts for a router, for example.

However when designing models have learnt - and been told - that it's dangerous to position things using joints. Because occasionally joints fail or become corrupted / confused. If one has built other parts of the design on top of elements that have been positioned using joints then the whole design can "fall apart". Particularly messy if projections were involved. That's why I was suggesting "capturing" the position and deleting the joint after it has done its job of aligning things. Did you never have an experience where joints in a model suddenly became confused?

[HughesTooling]

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@maker9876 wrote:

I guess after the Joint command one could use a Move command to achieve the final alignment and then a Capture Position. At that point the Joint could be deleted and would be no longer relevant to future operations, no longer a part of the timeline.

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Capture position should be avoided as much as possible. Joints should be easy to fix, a lot easier to keep all references correct than using move. Don't know if you'll ever use the CAM environment but I've seen lots of problems caused with move and save position. Also bad performance in general if the timeline is full of move and capture positions. Move might be OK for bodies but not for component and even when positioning bodies I'd use Translate or Point to Point not free move.

Mark

[HughesTooling]

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@maker9876 wrote:

Yes, I agree joints are a really nice way of positioning - and re-positioning - things. 

Really like to do that in CAM when laying out parts for a router, for example.

However when designing models have learnt - and been told - that it's dangerous to position things using joints. Because occasionally joints fail or become corrupted / confused. If one has built other parts of the design on top of elements that have been positioned using joints then the whole design can "fall apart". Particularly messy if projections were involved. That's why I was suggesting "capturing" the position and deleting the joint after it has done its job of aligning things. Did you never have an experience where joints in a model suddenly became confused?

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I'd recommend building your design using joints then use derive to create a new design for CAM if you need to lay the parts out. Never had joints become corrupt, I guess a big design change might lose references but you should be able to redefine any lost reference, you just need to make sure the joint references point the same as when originally created.

Mark

[maker9876]

@HughesTooling  I mention "CAM" and there you are!! 😉

Thanks for this.

- my understanding was that "Capture Position" is OK if used sparingly. That it might, in some ways, simplify things by making position at a certain point in the Timeline an absolute rather than contingent upon a bunch of prior calculations to be re-computed.

- the thing about Joints is not that they can't be fixed but that that they seem to be sensitive to "big design changes". (Big design change and then suddenly half of the joints in the file turn yellow. Panic.) Whereas a move / capture position doesn't seem to care so much about that. (That being said in the past may have created some of my own problems by not having 100% of sketches 100% constrained....). 

- mentioned CAM because when we reach the stage when joints are used to lay out shapes in stock on a router bed - or parts in a fixture or machine vice - then there's no design complexity to speak of and as such the file is likely to be stable. And if something were to go wrong at this last step of the process well it would be easy to put it right. No projected geometry nightmares....

- have just done a bunch of research on "Derive" which was not aware of. Very exciting.

- this lead to reading the contents of the green box : http://help.autodesk.com/view/fusion360/ENU/?caas=caas/discussion/t5/Fusion-360-Design-Validate-Docu...

- in the past have often started off with first version mechanical designs being created top-down within a single file. Then, when have an idea of what a single component should be like, going of and designing it from dimensioned sketches in a separate file and inserting it back into the original assembly. a) In order to make the final assembly more stable by eliminating all contingencies and calculations; b) with a view to being able to insert that individual component (if necessary multiple times) into a file for CAM with custom stock material / fixture etc.  Having read the aforementioned green box not sure that will change doing that but Derive is certainly sometimes going to be handy.

- coming back to the original topic of this thread it kind of feels like the Move command should allow one to select a line or axis on a component and "align it" with a line or axis elsewhere in the design. But perhaps I'm being geometrically naive?

Thanks again!

[HughesTooling]

The problem with capture position is it saves the position of all components at that point, a save with a few components at the start of the timeline might be ok but move the components again, add 50 more and there's a lot of info to save. Sometime you can have multiple orientations of a component saved as well and I've seen problems where the CAM losses the orientation of components and doesn't pickup modifications. Not in my designs, just problems people have uploaded to the forums.

Are the designs you're working on something that allows movement or static? I design mould tools so I tend to ground everything and design inplace as much as possible. If I use inserted parts I position with a joint, I wouldn't even notice if move was removed from Fusion, just don't like the way it works. Originally Move was not parametric in any way so joints just worked better. Are you following @TrippyLighting's advice on Rule #1, making components as self contained as possible and not using create components from bodies?

As for Derive, as all I'm doing is importing finished parts and very little design work is done in the CAM file the performance is good. In the past I found Fusion got very slow after a certain point, partly down to the amount of components and length of timeline but I also think references between the Cad and Cam become a problem. Another advantage with derive is only the components you are machining need to be derived, no need to bring in all the standard part like screws etc.. I've made quite a few moulds this way now and the performance is far better than in the past before derive was introduced.

Mark

[davebYYPCU]

However when designing models have learnt - and been told - that it's dangerous to position things using joints. Because occasionally joints fail or become corrupted / confused.

Not been my experience, totally the opposite.

Some one in authority told you that? 

Did you find out why the models are corrupted / confused, so the cause could be avoided?

[maker9876]

@HughesTooling  yes I use static and moving joints. And in the past used to use the static joints for positioning things whenever there was anything to positioned. (And in a file dedicated to CAM - without much in the way of design work going on, still do that).

@davebYYPCU  yes it was someone of authority in this forum (don't remember who!) who told me not to use joints for idle positioning. It's not that joints themselves corrupt so much as, if corruption creeps into the file, joints may be one of the first things to complain. And if they were used to position things which in turn were used for projected geometry then one can end up in a pretty irrecoverable mess. So I try to discipline myself to:

a) when linking in a component to position it using the move that comes at the moment of linking. Easy if you've imported a wheel and just have to move it to the centre point of the axle. Then use As Built Joint.

b) when positioning a component that was created within the file but is not in the right place (perhaps you created a wheel and then created copies for the 3 other axles), use the move command - ideally point to point or similar - to get it into place. Then As Built Joint.

As for what causes corruption, fully admit in the past have created problems with sketches that are not fully constrained. Also working on a file over many versions / generations of Fusion might not be a great thing to do. On a regular basis there are quirks that makes one think "uh oh... is something about to happen?" Have some projected geometry from a solid body that does not show up as a "surface". Divide the closed geometry with lines and discover that, right in the middle of the curve, there is some kind of invisible imperfection. Create a "fix" with my own line that won't in any case show up in the 3d print. But then the extrusion that I'll make from that surface will have various operations performed upon it and become integral to the design. It's easy to see how this might all unravel at some point. (This was the day before yesterday.) So I'm constantly on the defensive thinking what will happen IF things go wrong. 

[davebYYPCU]

(don't remember who!) who told me not to use joints for idle positioning.

I am not familiar with Idle positioning

a) when linking in a component to position it using the move that comes at the moment of linking. Easy if you've imported a wheel and just have to move it to the centre point of the axle. Then use As Built Joint.

b) when positioning a component that was created within the file but is not in the right place (perhaps you created a wheel and then created copies for the 3 other axles), use the move command - ideally point to point or similar - to get it into place. Then As Built Joint.

Two good reasons the file gets corrupted. 

Design Dependant of course, as likely was the advice you received.

As Built Joints are not parametric, should only be used when their Components are not going to be edited.

In option b), why would you Move, then As Built Joint, over a normal Joint without the move?

Normal Joints are parametric.

Simple example with the wheel and axle, 

Task - The shaft is to remain flush with the wheel when assembled.

Place both parts in position, and Create As built Joint - 

now edit the shaft length where the wheel is. 

Might help....

[maker9876]

Was kind of hoping someone from Autodesk might step in and clarify best practices.... 😉

[TrippyLighting]

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@maker9876 wrote:

However when designing models have learnt - and been told - that it's dangerous to position things using joints. Because occasionally joints fail or become corrupted / confused. 

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The occasional bug does not generally make a best practice "dangerous". Using joints is a best practice.

In my experience interfacing with users and analyzing designs many of them really don't fully understand the joint system in Fusion 360 and that also often leads to joints seemingly having randomly.